Bit is longer than dust shoe brush

[adam058]

I have the Axiom Dust Collection kit on my AR8 Pro but I'm using a longer plastic cutting bit for HDPE and the bit goes down lower than the brush, and it's making a big mess. I see there are longer brushes available on Amazon - can I buy another white plastic shoe brush frame? I guess I could try cutting one myself out of hdpe

What's the best solution here?

[dadealeus]

Mar 17, 2022 13:22:40 GMT -5 adam058 said:

I have the Axiom Dust Collection kit on my AR8 Pro but I'm using a longer plastic cutting bit for HDPE and the bit goes down lower than the brush, and it's making a big mess. I see there are longer brushes available on Amazon - can I buy another white plastic shoe brush frame? I guess I could try cutting one myself out of hdpe

What's the best solution here?

I understand the frustration. HDPE chips should be nice and large though - not any sort of fine shavings. If you're getting fine shavings, you need to slow your spindle or increase your feed rate. The large chips won't stick to your ball-screws or anything so you don't have to worry about them damaging your bearings by getting jammed into them.

As to taking care of the chips, you'll be hard-pressed to find a dust brush for long bits - the physics of it just don't work well enough. One solution I use for HDPE, specifically, is a chip fence:

Take a long strip of cardboard about 4" wide and tape it into a loop and then place it around your workpiece. It will catch most of the chips that fly off and keep them on top of your table. The cardboard ensures that if your machine accidentally runs into it, it's not going to hurt anything.

Other than that, you can stand there and manually handle the chips with a dust vac or your hose, but I haven't figured anything else out that works reliably enough.

[dadealeus]

Mar 17, 2022 13:22:40 GMT -5 adam058 said:

I have the Axiom Dust Collection kit on my AR8 Pro but I'm using a longer plastic cutting bit for HDPE and the bit goes down lower than the brush, and it's making a big mess. I see there are longer brushes available on Amazon - can I buy another white plastic shoe brush frame? I guess I could try cutting one myself out of hdpe

What's the best solution here?

Here's an example of what the chips should look like (around 20 seconds into the video, below) - though yours would probably be smaller (these are coming from a 1.5" surfacing bit). This video is from one of the first runs of my new machine (needed one with a larger footprint than Axiom offers to handle sheet goods).

This piece, in particular, is a 4'x8'x3.5" chunk of solid HDPE (around 650lbs.). The new machine has a 7.5hp spindle which chews through that HDPE without any issues - as you can hear in my excitement haha:

[adam058]

Interesting, thanks. I'll definitely try out the cardboard wall.

I'm running a 1/4" O flute, 1.5" flute, at 98in/min and 18k rpm. Do you think I should try slowing down the spindle and see how it goes?

Here's a pic of my chips:

photos.app.goo.gl/GUiqHPpCp9ejzNqm6

[dadealeus]

In general, running some tests, for a feed rate of 100 ipm, I'd reduce your depth of cut and cut that spindle speed almost in half.

Try this:

- Make sure your tool has as little stickout as possible (this helps to avoid tool deflection with higher chiploads and even small amounts of stickout can have a large effect on chatter). Obviously, don't place the cutting flutes into the collet, but choke up as much as possible.

- Make sure your workpiece is held very securely. It looks like you're bolting it directly to the t-slots, so that's great.

For your path:

- If at all possible, use adaptive clearing paths (not available in vectric). If you can't, you're not going to be able to push your cuts as hard because of the slot cuts and corners taking on a much higher chipload than the rest of your cuts).

- Ramp your toolpaths into the stock. A plunge and then straight to lateral movement at full depth of cut is going to be very hard on your tool and could easily snap it off if it's carbide (speaking from experience. I literally sheared off 7 tools last week while testing the limits of my new machine).

1) Feed rate of 100 IPM
2) Depth of cut to .25" (100% of your tool width)
3) Stepover to .1" (40% of your tool width)
4) Lower Spindle speed 10,000

Those values are pretty conservative, but should give you some decent chips. Adjust the speed as needed to get a good chip size (you can probably drop the speed slightly, but I wouldn't go below 9k or so for this particular cut. With HDPE, you should be able to almost roll the chips around in your hand like small pieces of gravel if you took a handful of them.

Your cut should have a nice hum to it without whining or rattling (chatter).

Once you're happy with chip size and cut quality/sound, you can try to push your productivity up by slowly increasing your depths of cut on each subsequent cut until you start hearing chatter (your cut edges will have ridges along them). If you'd like to keep pushing depth of cut at that point, back off on your stepover some, but I wouldn't go below about a 20% stepover for HDPE.

Finally, a note regarding finish quality - if you're using climb cutting, you're generally going to leave fuzzies (little pieces of plastic) along your cuts. Conventional milling is harder on your machine because the chip width increases as the cutter passes through the material (so you may have to run your speeds a bit more conservatively), but will give you cleaner edges when cutting in HDPE.

[dadealeus]

EDIT: I just realized I'm still climb milling in this video. I didn't realize it because I was taking such large bites, so the edges were going to be clean anyway. However, this is just a clearing pass - not a finishing pass (as you can see by the surface finish on the floor of the cut). You still need to run a finishing pass to clear that last bit of material and make a nice clean edge. If you run a climb cut in HDPE while taking small amounts of material, you're going to leave frayed edges (like you would in plywood). Conventional cuts on your finishing pass will prevent that.

Here's a video of those exact settings I just took (because cutting HDPE is incredibly satisfying):

[bentley]

How do you like the Avid in regards to the electronics and their spindle? I’m thinking of using the Axiom mechanicals and swapping out the electronics (steppers etc.)

[Gary Campbell]

I have heard of a number of users that have upgraded to Centroid Acorn, WinCNC and even UCCNC, but not Avid's Mach4 setup. I have even done a few of them in my shop. You may not have to change out anything but the controller/IO board. Some (read as most) will allow a direct DB25 connection to the existing IO board.

[dadealeus]

Mar 17, 2022 20:05:10 GMT -5 bentley said:

How do you like the Avid in regards to the electronics and their spindle? I’m thinking of using the Axiom mechanicals and swapping out the electronics (steppers etc.)

That's a really interesting idea.

The Avid setup is not without its flaws and, with shipping delays the way they are right now, it may take you several months to get the parts in (it took me around 6 months to receive my kit after placing the order).

The steppers are great (I opted for the NEMA 34s - lots of torque and a good max travel speed), but steppers are pretty much steppers. Their control box makes things nice to physically manage and the cables attach securely, though you would need to mount the control box somewhere or lay it on its side as the cables all come out of the sides and bottom of the box.

My only real complaint would be in the Mach software. It works well, but lacks some of the niceties that seem like "no-brainers". For example, if you press the "goto work origin" button, it immediately rapids toward the origin, but without lifting the spindle first. So, if you forget to do it manually after your cut and you have a clamp or something in the way, it'll snap your bit right off. I have yet to do this, thankfully, but I did take a chunk out of one of my plastic clamps I was using.

It also doesn't warn you very effectively if software limits are set or not. Once you home the machine, it sets up software limits to ensure your rapid movements don't slam into the physical limits of the machine. However, there are a number of things you can do that cause the software to lose the status of being properly homed - even though it should maintain that status. So, 3 or 4 times, I've though the machine was homed and made a rapid movement to one side or another (at 1000 IPM) and slammed the gantry into the sensors and steel plates.

On the flip side, the Mach software does let you pause and resume jobs much more easily than the Axiom machine does. With Mach, I can literally stop a job at any point, move the spindle, change tools, replace clamps, or whatever, then resume the program at the exact same location. I could even stop a job, load a different job, make that cut, and then come back to the previous job (as long as I didn't change my origin or if I set it back to exactly the same place).

You can also change (in detail) all the curves for your steppers (max travel, acceleration, etc.). I know you can also do that on the Axiom machine, but in Mach, you get nice visual graphs to represent your selections, etc.

Finally, Mach is also compatible with automatic tool changers if you want to add one to your machine.

So, I'd say it's a trade-off. I like a lot of the "safety" features on the Axiom firmware, but I also like the flexibility of Mach. It would be nice to have both in one package, but I guess that's just too much to ask for.

[dadealeus]

I wanted to include this, too. I cut that same square with an adaptive clearing path generated using Fusion 360. This path allows me to run much faster and at the full depth of cut in a single pass. Here are the changes:

You may be able to use these numbers with a pocket clearing path, but you're likely to get some bad stuff happening in the corners (chatter, maybe melting of the plastic).

Feed: 180 ipm

RPM: 18,000

Depth of Cut: 0.5" (200% of cutter diameter)

Stepover: 0.05" (20% of cutter diameter)

This will shoot chips all over your factory, but gets you a pretty quick clear while utilizing more than just the tip of your cutter (thereby prolonging your tool life):

[bentley]

Thanks for letting me know this. Have you asked someone at Avid if there is anywhere in the settings to raise the spindle before it traverses to the job start. I know for instance with the Axiom you can change these settings via the handheld. On my ShopSabre which runs a version of WINCNC it does all that automatically so as to prevent damage.
I’m only trying to have a possible quick fix if the Axiom’s electronics go for a dump. Then again you mentioned 6 months to receive your Avid kit. I don’t need both my machines to be running all the time but I’m getting larger and larger orders and I’m needing my Axiom to take up more of the load. So in a sense I’d have a hybrid machine. Frame and mechanical’s Axiom, electronics Avid.

[adam058]

Mar 17, 2022 15:50:33 GMT -5 dadealeus said:

In general, running some tests, for a feed rate of 100 ipm, I'd reduce your depth of cut and cut that spindle speed almost in half.

Try this:

- Make sure your tool has as little stickout as possible (this helps to avoid tool deflection with higher chiploads and even small amounts of stickout can have a large effect on chatter). Obviously, don't place the cutting flutes into the collet, but choke up as much as possible.

- Make sure your workpiece is held very securely. It looks like you're bolting it directly to the t-slots, so that's great.

For your path:

- If at all possible, use adaptive clearing paths (not available in vectric). If you can't, you're not going to be able to push your cuts as hard because of the slot cuts and corners taking on a much higher chipload than the rest of your cuts).

- Ramp your toolpaths into the stock. A plunge and then straight to lateral movement at full depth of cut is going to be very hard on your tool and could easily snap it off if it's carbide (speaking from experience. I literally sheared off 7 tools last week while testing the limits of my new machine).

1) Feed rate of 100 IPM
2) Depth of cut to .25" (100% of your tool width)
3) Stepover to .1" (40% of your tool width)
4) Lower Spindle speed 10,000

Those values are pretty conservative, but should give you some decent chips. Adjust the speed as needed to get a good chip size (you can probably drop the speed slightly, but I wouldn't go below 9k or so for this particular cut. With HDPE, you should be able to almost roll the chips around in your hand like small pieces of gravel if you took a handful of them.

Your cut should have a nice hum to it without whining or rattling (chatter).

Once you're happy with chip size and cut quality/sound, you can try to push your productivity up by slowly increasing your depths of cut on each subsequent cut until you start hearing chatter (your cut edges will have ridges along them). If you'd like to keep pushing depth of cut at that point, back off on your stepover some, but I wouldn't go below about a 20% stepover for HDPE.

Finally, a note regarding finish quality - if you're using climb cutting, you're generally going to leave fuzzies (little pieces of plastic) along your cuts. Conventional milling is harder on your machine because the chip width increases as the cutter passes through the material (so you may have to run your speeds a bit more conservatively), but will give you cleaner edges when cutting in HDPE.

Thanks! I'll start experimenting